Threaded Hole Not Deep Enough After Processing: How to Fix It
A threaded hole not deep enough shows up at assembly, not at the machine. This page maps each symptom to its real cause and gives the rework or redesign that actually holds. Written for process engineers and buyers who have to close the issue on the floor.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
Symptom, likely cause, and what to do
Match the row to what you see at assembly, not to what you assume happened at the machine.
| Symptom | Likely cause | Action |
|---|---|---|
| Bolt bottoms out, thread still open | Tap drill stopped short of drawing depth | Measure remaining depth, re-drill deeper if wall allows |
| Screw enters 3 turns then stalls | Bottoming tap not run to full depth | Run a bottoming tap, recheck with a plug gauge |
| Gauge goes in, screw does not | Thread depth is fine, head clearance is not | Check counterbore and washer stack height |
| Depth reads correct, bolt still short | Usable thread is less than drilled depth | Recompute usable depth from chamfer and lead |
| Threads tear near the bottom | Chip packing in a blind hole | Reduce peck depth, add through-coolant or MQL |
| Only some parts fail | Drill wear or thermal drift on a long run | Track drill life, re-measure first article each shift |
| Hole breaks into a cavity or slot | Drawing started from the wrong face | Rework with a deeper pilot or weld-repair boss |
Fix the depth, then fix the drawing
Re-drill and bottom-tap when wall thickness allows. Use an insert when it does not. If the same part keeps failing, the drill depth on the drawing is wrong, not the operator.
Why a threaded hole ends up shallower than the drawing
The number on the drawing is usually full thread depth, not drilled depth. Those are two different values and the gap between them is where most short-thread problems live. A tap cannot cut usable thread up to the very bottom of the hole. The chamfer at the entry and the lead-in taper at the tip both consume axial length before the first full-form thread appears.
For a standard spiral point tap, the lead is roughly 3 to 5 pitches. That length produces partial thread, not full thread. For a bottoming tap, the lead drops to about 1 to 1.5 pitches. So if the drawing calls for M6 full thread at 15 mm deep, the drilled hole has to go past 15 mm by at least the lead, plus a small clearance margin for chips.
Thread pitch matters more than people expect. At M6 × 1.0, one pitch is 1 mm. At M16 × 2.0, it is 2 mm. Multiply by lead length and the same drawing tolerance turns into very different drill depths. On coarse threads in deep holes the required drill depth can exceed the wall thickness you have available.
The drilled depth also has to account for the drill point angle. A 118° point leaves a cone at the bottom, and that cone is not usable thread. On a Ø5 mm tap drill, the cone adds roughly 1.5 mm of dead depth. If the programmer set the drill depth equal to the thread depth, the hole is already short before tapping starts.
- 1Drilled depth ≠ thread depthAdd lead length plus point cone plus a 1–2 mm chip margin.
- 2Bottoming taps recover 2–4 mmUseful when you cannot drill deeper because of wall thickness.
- 3Check which face the depth is fromA 0.2 mm face mismatch shifts the whole stack.
Process causes: welding, datum shift, and programming
A welded assembly is a common trigger. If the threaded hole is machined before welding and the end face is milled after, the face moves. The thread stays where it was. Now the bolt has to travel through a thicker stack and the thread runs out early. The fix is sequence, not tolerance: drill and tap after the final face cut, or leave stock on the face and finish it in the same setup as the thread.
Datum shift is quieter. A part flipped for second-op machining inherits the flatness and burr condition of the first face. If that face is not clean, the drill starts from a false zero and stops short by the difference. On a 4,000 mm maximum processing size part, a 0.3 mm face variation is easy to miss and hard to see on a height gauge.
Programming errors cluster around three habits: entering drill depth as thread depth, forgetting the point cone, and using absolute depth from the wrong Z zero. On mill-turn centers and 5-axis work, a rotated workplane can flip the sign of the depth value. The hole looks correct in simulation and comes out shallow in metal.
Tool wear is the slow version. A drill that has run 400 holes is shorter in effective reach than a new one after regrinding. If the drill is re-pointed with a steeper angle, the cone gets longer and the usable depth shrinks again. Track drill life by hole count, not by calendar.
- 1Weld-after-threadRemachine the face and re-cut the thread in one setup.
- 2False zero from a burred faceDeburr the datum face before the second operation.
- 3Regrind changes the point angleRe-post the drill depth after every regrind.
When a shallow thread is usable and when it is not
Usable thread length, not drilled depth, sets the joint strength. For a steel bolt in an aluminum part, a common rule is that engagement of 1.5 times the nominal diameter carries most of the load. At 2 times the diameter, additional thread adds little. For a steel bolt in steel, 1 to 1.5 times the diameter is often enough. Below 1 times the diameter, the threads strip before the bolt yields.
That rule is a starting point, not a pass. Load direction changes it. A thread in tension is more forgiving than one in shear or one that sees vibration. A threaded hole in a die-cast boss, where the material is ADC12 or AZ91D, needs more engagement than the same thread in 4140 steel because the parent material yields first.
Wall thickness is the other limit. If re-drilling deeper would leave less than one thread diameter of material around the hole, the boss will bulge or crack during tapping. In that case, deeper is not safer. You either accept the shorter engagement with a longer bolt and a spacer, or you move to a threaded insert.
Threaded inserts change the calculation. A keylocking or helical insert spreads load over more material and lets you use a shorter hole. For a threaded hole not deep enough in a soft alloy, an insert is often cheaper than scrapping the part, provided there is enough boss for the insert's outer thread.
- 11.5 × diameterTypical target for steel screws in aluminum.
- 2Below 1 × diameterStrip risk before bolt yield. Do not ship as-is.
- 3Keep one diameter of wallLess than that and the boss deforms during tapping.
Rework routes and what each one costs you
Re-drill and re-tap is the first option and the cheapest when geometry allows. You need the original hole to be concentric with the new one, and you need wall thickness left after the deeper cut. Run the drill 0.05–0.10 mm under the nominal tap drill if the existing hole is already threaded, because the drill will follow the old path. Then run a bottoming tap to the new depth.
Helical inserts work when the hole cannot grow outward, only inward. Drill out to the insert's STI tap drill size, tap, and install. The result is a stronger thread in soft material, but you lose the ability to use the original fastener size unless the insert matches it. Check that the boss diameter still has 0.5 times the insert outer diameter of wall.
Weld repair is the last resort and it is not free. Filling a threaded hole and re-machining it changes the local material properties. On 6061-T6 or 7075, welding drops the heat-affected zone strength and you may not get it back with a re-heat-treat if the part is large. Use it for low-stress bosses only, and re-cut the face after welding.
The fourth route is design change: a longer bolt with a spacer, a through-bolt with a nut, or a relocated hole. It is not a shop fix, but it is often the only one that holds on a thin-walled casting. If three of the previous options fail on the same part number, the drawing is the problem.
- 1Re-drill and bottom tapCheapest. Needs wall thickness and concentricity.
- 2Helical insertBest for soft alloys. Watch the outer thread size.
- 3Weld and remachineLow-stress bosses only. HAZ strength drops.
Step by step: diagnose and fix a shallow threaded hole
- 1Measure the hole, not the boltUse a depth gauge or a pin with a known length. Record drilled depth, thread depth to the last full form, and the remaining cone. Write all three values down before touching the program.
- 2Compute the missing lengthMissing length = required full thread − measured full thread. Add 1–2 mm for chip clearance and, if the tap is a spiral point type, 3–5 pitches of lead. This is the extra drill depth you need.
- 3Check wall thickness before drilling deeperKeep at least one thread diameter of material around the hole. On a Ø6 mm thread, that means 6 mm of wall. If you do not have it, stop and go to the insert route instead.
- 4Re-drill with a stub or reduced-shank drillRun 0.05–0.10 mm under the standard tap drill if the hole is already threaded. Peck 1 × diameter per pass, and use through-coolant or MQL to clear chips from the blind end.
- 5Tap with the right style for the depthSpiral flute for blind holes in aluminum and brass. Spiral point for through holes. Bottoming tap for the last 2–4 mm. Target 60–70% thread engagement, not 100%.
- 6Verify with a plug gauge and a real boltThe gauge checks thread form. The bolt checks clearance through the whole stack. Do both, because a gauge can pass while the joint still fails on head clearance.
- 7Update the drawing and the programIf the fix worked, change the drill depth in the CAM file and note the lead allowance on the drawing. Otherwise the same short hole ships on the next run.
Questions engineers ask about shallow threads
How much deeper should the tap drill be than the thread depth?
Add the tap lead, the drill point cone, and a chip margin. For a spiral point tap at M6 × 1.0, the lead is about 3–5 mm. A 118° point on a Ø5 mm drill adds about 1.5 mm of cone. A 1–2 mm chip margin keeps the bottom clean.
Total: drill depth is typically 5–8 mm deeper than the required full thread depth on a small metric thread. On coarse threads like M16 × 2.0, it can be 12 mm or more.
Can I just use a longer bolt instead of reworking the hole?
Sometimes. If the existing full thread is at least 1.5 times the nominal diameter and the bolt reaches it, the joint is usually fine. If engagement is below 1 times the diameter, a longer bolt does not help because there is no thread for it to grip.
Check clearance too. A longer bolt may bottom in the hole or interfere with the mating part.
Why does the depth check pass but the screw still stops short?
The depth check usually measures drilled depth or thread depth. The screw needs clearance for its full length, the washer, and any gasket. If the counterbore is shallow or the washer stack is thick, the screw runs out of travel before it reaches the thread.
Measure the assembled stack, not the hole alone.
Is a bottoming tap enough to fix a short blind hole?
It recovers 2–4 mm compared with a standard spiral point tap, depending on pitch. That is often enough. It does not create material where none exists, so if the drilled hole itself is short, you still have to drill deeper or switch to an insert.
What causes threads to tear at the bottom of a blind hole?
Chips. In a blind hole, chips pack at the bottom and the tap recuts them, which tears the thread form and raises torque. Reduce peck depth, use through-coolant or MQL, and back the tap out more often on deep holes.
A dull tap makes it worse. Replace taps on a hole count, not when they break.
When should we switch from re-drilling to a threaded insert?
When wall thickness rules out a deeper hole, or when the parent material is soft. Helical inserts in aluminum, magnesium, or die-cast alloys hold better than a deeper cut in thin material.
Check that the boss has enough diameter for the insert outer thread plus 0.5 times that diameter of wall.
Send us the drawing and the failed hole
We quote and return a free DFM analysis within 12 hours, with thread depth and drill depth called out separately. No minimum order quantity, from one prototype to 10,000+ part runs.
12-hour quote100% inspectionNDA on request
More machining notes
We publish setup notes, tooling trials and inspection data from the factory floor.
